Predefined Temperature
In stress/displacement analysis the temperature difference between a predefined temperature field and any initial temperatures (Initial Conditions) will create thermal strains if a thermal expansion coefficient is given for the material (Thermal Expansion). The predefined temperature field also affects temperature-dependent material properties, if any. In Abaqus/Explicit temperature-dependent material properties may cause longer run times than constant properties.
You define the magnitude and time variation of temperature at the nodes, and Abaqus interpolates the temperatures to the material points.
Input File Usage
Use the following option to specify a predefined temperature field:
TEMPERATURE
Abaqus/CAE Usage
Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step
Restrictions
Do not specify predefined temperature fields in a pure heat transfer analysis, a coupled thermal-electrical analysis, a fully coupled temperature-displacement analysis, or a fully coupled thermal-electrical-structural analysis; instead, specify a boundary condition (Boundary Conditions) to prescribe temperature degrees of freedom (11, 12, ...).
Predefined temperature fields cannot be specified in an adiabatic analysis step or in any mode-based dynamic analysis step.
To specify a predefined temperature field in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either initial temperatures (see Defining Initial Temperatures) or a predefined temperature field.